CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

MovingCone tutorial and icoDyMFoam with addingremoving mesh layers

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 6, 2007, 03:25
Default I would like to modify the mov
  #1
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 8
idosil is on a distinguished road
I would like to modify the movingCone tutorial to add/ remove mesh layers instead of changing mesh size. How do I do it? Is there an example, tutorial on setting dynamic mesh with topologic changes?
Where can I find info on using blockMesh to set sets and zones? I understand it is required in order to define topologic changes of the mesh.

Best regards, ido
idosil is offline   Reply With Quote

Old   September 6, 2007, 11:19
Default Try this: http://www.cfd-o
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Try this:

movingConeTopo.tgz .

You may need some of my bug fixes etc as well, but that will give you an idea of what the case should look like.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 8, 2007, 09:11
Default Thanks Hrv, It worked fine
  #3
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 8
idosil is on a distinguished road
Thanks Hrv,

It worked fine after a few small modifications. Now I have to work to understand the magic. Is there a demo with all the optional arguments to dynamicMeshDict file?

Best regards, Ido
idosil is offline   Reply With Quote

Old   September 8, 2007, 09:37
Default Actually, I am not too proud o
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Actually, I am not too proud of that class and tutorial. There are much better and more flexible examples, either moving a user-defined box using the scaling or automatic mesh motion for more complex cases.

You should look at:

- dynamicBodyFvMesh
Automatic motion of the mesh around a moving body. A direction,
amplitude and frequency of translational motion and origin, axis,
amplitude and frequency of rotational motion must be specified.

- dynamicBoxFvMesh
Automatic simplified mesh motion for "box-in-mesh" cases. Here,
a direction of motion is defined, together with motion amplitude
and frequency. The domain is separated into three parts, where
the middle part moves accordign to the prescribed motion law.
Parts of the mesh before and after the obstacle are scaled.

- dynamicMotionSolverFvMesh
Dynamic FV mesh, where a motion solver is used to move the mesh.
The user specifies motion using the boundary condition on the
appropriate motion variable.

As for the parameters, the best things is to look at the constructor. I usually do not hide the parameters, but you never know

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 18, 2007, 01:29
Default Boundary conditions for slidin
  #5
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 8
idosil is on a distinguished road
Boundary conditions for sliding interface

Dear Hrv,

I have been studying the various dynamic mesh solvers supplied with OpenFOAM. I am working now with movingValveLayersFvMesh and wrote a small test case for it (for icoDyMFoam solver). The model simulates a piston moving inside a cylinder, closing and outlet. The "insideSlider" patch boundary conditions should be wall (fixedValue (0 0 0)) where ever it is not attached to the "outsideSlider". Where they are attached it should be an internal boundary. When I set the boundary condition to fixedvalue it was so everywhere including where it is attached to the other patch. When I changed it to zeroGradient I get flow through the attaching zone but the velocity does not goes to zero on the "wall" zone. How can I get the required behavior?

Best regards, Ido

P.S. How does I attach a file to this post?
idosil is offline   Reply With Quote

Old   September 18, 2007, 01:35
Default Boundary conditions for slidin
  #6
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 8
idosil is on a distinguished road
Boundary conditions for sliding interface (with attachment)

Dear Hrv,

I have been studying the various dynamic mesh solvers supplied with OpenFOAM. I am working now with movingValveLayersFvMesh and wrote a small test case for it (for icoDyMFoam solver, see attached file). The model simulates a piston moving inside a cylinder, closing and outlet. The "insideSlider" patch boundary conditions should be wall (fixedValue (0 0 0)) where ever it is not attached to the "outsideSlider". Where they are attached it should be an internal boundary. When I set the boundary condition to fixedvalue it was so everywhere including where it is attached to the other patch. When I changed it to zeroGradient I get flow through the attaching zone but the velocity does not goes to zero on the "wall" zone. How can I get the required behavior?

movingValve.rar

Best regards, Ido
idosil is offline   Reply With Quote

Old   September 18, 2007, 10:01
Default Hi, I tested the model agai
  #7
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 8
idosil is on a distinguished road
Hi,

I tested the model again today with fixedValue boundary conditions on the sliding interfaces and it worked correctly.

Bye, Ido
idosil is offline   Reply With Quote

Old   September 18, 2007, 17:44
Default Sorry, don't get it - can you
  #8
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Sorry, don't get it - can you please confirm if this works OK or not. If there's trouble, I'll have a look (I've run it less than 2 weeks ago).

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 19, 2007, 12:11
Default Hi Hrv, 1) your model movin
  #9
New Member
 
Ido Silverman
Join Date: Mar 2009
Posts: 13
Rep Power: 8
idosil is on a distinguished road
Hi Hrv,

1) your model movingConeTopo works fine.

2) I have looked around and made a model to study the dynamic mesh solver movingValveLayersFvMesh. At first I had problem with boundary conditions on the sliding faces but later have been able to resolve it. The case is given in the attached file movingValve.tgz .

Bye, Ido
idosil is offline   Reply With Quote

Old   August 5, 2008, 03:12
Default Hi, I have a question about th
  #10
zhaolj98
Guest
 
Posts: n/a
Hi, I have a question about the movingConeTopo tutorial. This tutorial adds/removes mesh layers instead of changing mesh size.

When the current cell layer thickness exteeds the maxThickness setted in the dynamicMeshDict, the new added cell layer thickness is fixed to the maxThickness?

Can I choose another thickness, for example, 0.8*maxThickness, to add the new cell layer? If can, how can I do it?

By the way, I am using the OF-1.4.1-dev.

Thanks.

ZHAO
  Reply With Quote

Old   August 5, 2008, 03:37
Default Hi Have you tried to play a
  #11
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,592
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi

Have you tried to play around with the minThickness/maxThickness in

~/OpenFOAM/mekngj-1.4.1-dev/run/tutorials/icoDyMFoam/movingConeTopo/constant/dyn amicMeshDict

I suppose that is where you want to go.

/ Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   August 5, 2008, 04:16
Default You can use any thickness you
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
You can use any thickness you like. Just make sure that your motion and time-step are appropriate, so that you do not move for eg. 2 layer thicknesses in a single time-step.

Enjoy,

Hrv
hua1015 likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 5, 2008, 04:22
Default Hi, Niels. Maybe you did no
  #13
zhaolj98
Guest
 
Posts: n/a
Hi, Niels.

Maybe you did not understand my question.

I know that the min/maxThickness parameters are setted in the movingConeTopo/constant/dyn amicMeshDict. But in the codes of OF-1.4.1-dev, where is the new added cell layer thickness fixed to this maxThickness of the dynamicMeshDict?

When the current cell layer thickness exteeds the maxThickness of dynamicMeshDict, can I fix the new cell layer thickness to be any multiples of maxThickness by modifing the codes?

Thanks.

ZHAO
  Reply With Quote

Old   August 5, 2008, 05:13
Default Hi, Hrvoje. Thanks for your re
  #14
zhaolj98
Guest
 
Posts: n/a
Hi, Hrvoje. Thanks for your reply.

When the old master cell layer thickness exceeds the maxThickness, the new points are added. If the new points are added at the maxThickness away from the master zone points, a old slave cell layer whose thickness is equal to the maxThickness, and a new cell layer whose thickness is equal to (the old master layer thickness - maxThickness) will be created. If the old master cell layer thickness exceeds the maxThickness very slightly, the newly created layer may be very thin. The very thin cell layer is not good for the convergence.

However, if I fix the old slave cell layer thickness to be less than 0.8*maxThickness, the newly created layer thickness will be greater than 0.2*maxThickness, and will be not very thin. So, how can I introduce this 0.8 or any other value to the codes, so that a thin cell layer can be avoided neatly?

Thanks.

ZHAO
  Reply With Quote

Old   September 26, 2008, 11:01
Default Dear Prof Jasak We was starti
  #15
New Member
 
sonia esteban
Join Date: Mar 2009
Posts: 12
Rep Power: 8
gmc_salta is on a distinguished road
Dear Prof Jasak
We was starting to work with dynamic mesh. We began with icoDyMFoam of tutorial and work fine, but we need refined mesh in some place our domain (transient problem) and not in moving mesh.
We look some discussion on forum. One of them indicate that exits improved version of icoDyMFoam.

We download of this site http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/applications/solvers/incompressible/
all files of solver icoDyMFoam (by HJasak). Then we tried to compiled them, with version OF1.4.1, and it give this message:

Making dependency list for source file icoDyMFoam.C
could not open file initTotalVolume.H for source file icoDyMFoam.C
could not open file checkTotalVolume.H for source file icoDyMFoam.C
SOURCE=icoDyMFoam.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/dynamicFvMesh/lnInclude -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/dynamicMesh/lnInclude -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/meshTools/lnInclude -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/foam/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/icoDyMFoam.o
icoDyMFoam.C:45:32: error: initTotalVolume.H: No existe el fichero o el directorio
icoDyMFoam.C:56:37: error: checkTotalVolume.H: No existe el fichero o el directorio
make: *** [Make/linux64GccDPOpt/icoDyMFoam.o] Error 1

We search files initTotalVolume.H and checkTotalVolume.H, in home/usr/OpenFOAM/OpenFOAM-1.4.1 but no found them.
We copied checkTotalVolume.H of another solver (icoMeshMotionFoam) but we not sure that it's correct. Please, could you send us the correct files or indicated how to take them?
Thanks very much
Sonia and Ana
gmc_salta is offline   Reply With Quote

Old   September 26, 2008, 12:04
Default Ensure that you have the $(FOA
  #16
Senior Member
 
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 386
Rep Power: 15
deepsterblue will become famous soon enough
Ensure that you have the $(FOAM_SRC)/OpenFOAM/lnInclude directory added to your Make/options file. The files you're looking for exist there.
__________________
Sandeep Menon
University of Massachusetts Amherst
https://github.com/smenon
deepsterblue is offline   Reply With Quote

Old   September 29, 2008, 08:13
Default Hi, Sandeep Thank you for you
  #17
New Member
 
sonia esteban
Join Date: Mar 2009
Posts: 12
Rep Power: 8
gmc_salta is on a distinguished road
Hi, Sandeep
Thank you for your quick answer, our version OF-1.4.1, was updated at sep/07.
We look for the files and find them but we have another error,
>> cannot find -llduSolvers
Again search this file in

http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/src/

and we find all files that needed, we are compiled them now.

Regard and thank for your suggestion
Sonia y Ana
gmc_salta is offline   Reply With Quote

Old   September 30, 2008, 10:01
Default Hi, I start using openFoam le
  #18
wops
Guest
 
Posts: n/a
Hi,
I start using openFoam less than a month ago, version 1.5 and I'm not very familiarized with it.

I try to run movingValve and movingConeTopo but it didn't work.
I wanted to know if I have to install something previously to running the case or what do I do wrong

I'm the only one with this problem?
Thanks, René
  Reply With Quote

Old   September 30, 2008, 11:26
Default You have to be specific. Can y
  #19
Senior Member
 
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 386
Rep Power: 15
deepsterblue will become famous soon enough
You have to be specific. Can you post some output?
__________________
Sandeep Menon
University of Massachusetts Amherst
https://github.com/smenon
deepsterblue is offline   Reply With Quote

Old   September 30, 2008, 11:42
Default Ok, here are the outputs. S
  #20
wops
Guest
 
Posts: n/a
Ok, here are the outputs.

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 0.111111
Time = 0.111111

time:0.111111 curMotionVel_1.77987e-05 0 0) curLeft:-0.007 curRight:-0.0035
No topology change

Executing mesh motion

Attempt to return dictionary entry as a primitive

file: /home/wops/OpenFOAM/wops-1.5/run/movingConeTopo/system/fvSolution::U::preconditi oner from line 70 to line 70.

From function ITstream& primitiveEntry::stream() const
in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83.

FOAM aborting

#0 Foam::error::printStack(Foam:stream&) in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::IOerror::abort() in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::dictionaryEntry::stream() const in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#3 Foam::dictionary::lookup(Foam::word const&, bool) const in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/wops/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::fvMatrix<foam::vector<double> >::solve(Foam::Istream&) in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"
#6 Foam::lduMatrix::solverPerformance Foam::solve<foam::vector<double> >(Foam::tmp<foam::fvmatrix<foam::vector<double> > > const&) in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"
#7 main in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"
#8 __libc_start_main in "/lib/i686/cmov/libc.so.6"
#9 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/wops/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/icoDyMFoam"

thanks,
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
inflation layers for hexa mesh using icem cfd Apple CFX 4 January 6, 2012 01:12
Combined compressible flow and moving mesh with layers andersking OpenFOAM Running, Solving & CFD 4 March 1, 2011 10:40
Mesh Problem with icoDyMFoam yuhai OpenFOAM Running, Solving & CFD 5 January 14, 2009 15:57
Mesh Problem with icoDyMFoam yuhai OpenFOAM Running, Solving & CFD 0 January 12, 2009 18:53
Problem with icoDyMFoam tutorial matlie OpenFOAM Bugs 10 April 26, 2007 04:51


All times are GMT -4. The time now is 16:14.